How to model a parametric hook?

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Christoph
Posts: 54
Joined: Fri Jul 08, 2016 9:02 pm

Re: How to model a parametric hook?

Postby Christoph » Sat Apr 21, 2018 1:19 pm

Hi,

sorry for the late response, working week was quite busy. Here ist the original FreeCAD file (outdated now)
Attachments
FreeCAD Tutorial - Wie modelliert man einen Haken.FCStd
(636.21 KiB) Downloaded 36 times
Last edited by Christoph on Sat Apr 21, 2018 1:33 pm, edited 1 time in total.
Christoph
Posts: 54
Joined: Fri Jul 08, 2016 9:02 pm

Re: How to model a parametric hook?

Postby Christoph » Sat Apr 21, 2018 1:28 pm

@Wilfried: I tried curves Workbench, but decided to keep the whole modeling process within Part Design next to avoid problems mixing different workbenches. To improve the look of the sweep, I changed the whole design by using a loft between the transition of the eyelet and the sweep. Furthermore, I used B-Splines instead of the slot-tool. The sweep is not perfect, but much better then before and the whole body doesn't have the ungly plane sufaces on the eyelet.

Especially the placing of Datum-Planes is now much more professional!

I attach the new file.

I recorded a new video, which can be found here:
phpBB [video]


OS: Windows 10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.13532 (Git)
Build type: Release
Branch: master
Hash: 4adeb7702da610da2c7f3014217044167109f0d6
Python version: 2.7.14
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.2.0
Locale: German/Germany (de_DE)
Attachments
Haken.FCStd
(439.22 KiB) Downloaded 35 times
dbecad
Posts: 80
Joined: Fri Mar 16, 2018 11:10 pm

Re: How to model a parametric hook?

Postby dbecad » Sat Apr 21, 2018 4:27 pm

Thanks Christoph for that great educational video.
Following it without sound is easy enough, google auto-subtitle + auto-translate is pretty funny (pun intended), as in you kept using the "laughing tool" :lol:

While I'm trying to reproduce, I run into issues with the loft:
- the first point used seems to be off ans thus the result is twisting, is there a way to avoid it
- the loft is not following the tangent of the ring (not smooth), I don't see any options to tell it to follow the original surface

Your result on the left, mine on the right.
loft.png
loft.png (82.52 KiB) Viewed 851 times
Thanks for you help and tips.
Cheers!

----------
OS: Ubuntu 16.04.4 LTS
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.13548 (Git)
Build type: None
Branch: master
Hash: 32973995423007a59cd18799c63383150811d1a7
Python version: 2.7.12
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.2.0
Locale: English/UnitedStates (en_US)
Attachments
hook.fcstd
(81.42 KiB) Downloaded 30 times
Christoph
Posts: 54
Joined: Fri Jul 08, 2016 9:02 pm

Re: How to model a parametric hook?

Postby Christoph » Sun Apr 22, 2018 6:02 pm

Hi dbcad,

I applied constraints to all the sketches in your file and the loft worked out. But I coudn't find the solution why the loft wasn't working on your original file.
Regards
Christoph
Attachments
hook.fcstd
(126.61 KiB) Downloaded 28 times
freecad-heini-1
Posts: 7038
Joined: Tue Jan 07, 2014 11:10 am
Contact:

Re: How to model a parametric hook?

Postby freecad-heini-1 » Sun Apr 22, 2018 7:38 pm

Christoph wrote:
Sun Apr 22, 2018 6:02 pm
Hi dbcad,

I applied constraints to all the sketches in your file and the loft worked out. But I coudn't find the solution why the loft wasn't working on your original file.
Regards
Christoph
I can tell you why it's going wrong. All sketches must have the startpoint at the same side. So you have to move the two sketches under 90° in the sketcher, so please delete the vertical constraint, rotate with the mouse and then set a new vertical or horizontel constraint, and dimension the elipse. Then you will see that the loft will work.
dbecad
Posts: 80
Joined: Fri Mar 16, 2018 11:10 pm

Re: How to model a parametric hook?

Postby dbecad » Mon Apr 23, 2018 4:29 am

Thanks Christoph for your check and confirming my problem!
freecad-heini-1 wrote:
Sun Apr 22, 2018 7:38 pm
I can tell you why it's going wrong. All sketches must have the startpoint at the same side. So you have to move the two sketches under 90° in the sketcher, so please delete the vertical constraint, rotate with the mouse and then set a new vertical or horizontel constraint, and dimension the elipse. Then you will see that the loft will work.
Thanks Heini, that is what i kind of figure out when looking at the "seam line on the surface" and reading how the loft was working (https://www.freecadweb.org/wiki/Part_Lo ... al_Details), the problem is that these ellipses have a dominant (larger) axes so to get similar shape as Christoph I cannot really turn 90degrees and get the same aspect ratio.
Maybe, would it be possible to define a % from the first point for the location of the seam for each slice instead of relying on the "random" location of this first point? I could submit a ticket if you think it's a worthy feature. I feel that the current loft is a bit restricted right now.
Thanks!
Cheers
chrisb
Posts: 25211
Joined: Tue Mar 17, 2015 9:14 am

Re: How to model a parametric hook?

Postby chrisb » Mon Apr 23, 2018 7:30 am

dbecad wrote:
Mon Apr 23, 2018 4:29 am
the problem is that these ellipses have a dominant (larger) axes so to get similar shape as Christoph I cannot really turn 90degrees and get the same aspect ratio.
Maybe, would it be possible to define a % from the first point for the location of the seam for each slice instead of relying on the "random" location of this first point? I could submit a ticket if you think it's a worthy feature.
My guess is that the seam comes from the OCC kernel and FreeCAD cannot change it. So it's not worth a ticket. If you need more control over the elliptical segments you have to divide the ellipse itself into different pieces.
Jee-Bee
Posts: 2027
Joined: Tue Jun 16, 2015 10:32 am
Location: Netherlands

Re: How to model a parametric hook?

Postby Jee-Bee » Mon Apr 23, 2018 7:47 am

In old features of creo related probles exist with circular or elipse that it don't know where to cut the sketches. so you have to do it youreself in the sketch...
dbecad
Posts: 80
Joined: Fri Mar 16, 2018 11:10 pm

Re: How to model a parametric hook?

Postby dbecad » Mon Apr 23, 2018 3:18 pm

Thanks all for your comments,
so for future reference, I changed the ellipses to splines and then manually aligned the first points (top right) to get the correct result (bottom right, the seam is straight).

I understand FC might not control the first point, but it does make figuring out where that point is on a curve difficult. You have to exit the sketch mode to see it (unless I missed an option?) and the first point of the ring bottom face is what looks like a single black pixel on my screen (see left screen-shot).
Could we have an option to mark first point more visibly maybe?
Cheers
loft2.png
loft2.png (113.66 KiB) Viewed 760 times
------------------
OS: Ubuntu 16.04.4 LTS
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.13559 (Git)
Build type: None
Branch: master
Hash: 68f25713d3802b2bafef13877417ba2a416bb929
Python version: 2.7.12
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.2.0
Locale: English/UnitedStates (en_US)
Attachments
hook.fcstd
(83.82 KiB) Downloaded 37 times